• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Community Forums
  2. Custom IC SKILL
  3. ADE simulation files -- error

Stats

  • Locked Locked
  • Replies 6
  • Subscribers 144
  • Views 3073
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

ADE simulation files -- error

Thodoros
Thodoros over 14 years ago

 Hello,

I am trying to assign a simulation file to a ADE run (ADE ->setup -> simulation files) which contains the simple that follows:

simulator lang=spectre
_vAddr\<3\> (Addr\<3\> 0) vsource val0=0 val1=0 period=500p width=250p type=pulse

 I have ic6.1.4 and when I execute "Netlist and Run" I get the following error:

 Error found by spectre during circuit read-in.
     ERROR (SFE-874): "/home/simop/simulation/sram_PCCA/spectre/schematic/netlist/stimuli/stem" 2: Unexpected operator "<".

What really happens is that at the ~/ ... /simulation/<design>/schematic/netlist/stimuli/ directory the copied stimuli file has errased the "\" character.

I really have to add that character and perform ADE ->Simulation ->Run in order to continue with the simulation.

Can I ovefrcome this?

Thanks,

Thodoros

  • Cancel
  • Thodoros
    Thodoros over 14 years ago

     OK I found a walk aroud.

     

    Instead of writing the stimuli

    simulator lang=spectre
    _vAddr\<3\> (Addr\<3\> 0) vsource val0=0 val1=0 period=500p width=250p type=pulse

     

    I add an extra "\" and the stimuli

    simulator lang=spectre
    _vAddr\\<3\\> (Addr\\<3\\> 0) vsource val0=0 val1=0 period=500p width=250p type=pulse

     is OK

    Is this the proper way of writing stimuli files?

    Thanks,

    Thodoros

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • Andrew Beckett
    Andrew Beckett over 14 years ago

    The stimulus file goes through a mapping process which allows "schematic" names to be used via the [#...] syntax. These get mapped into whatever was used in the netlist (via mapping). So you'd use something like this:

    v1 ([#bus<0>] 0) vsource type=sine freq=1M ampl=1
    v2 ([#bus<1>] 0) vsource type=sine freq=2M ampl=1.5
    v3 ([#bus<2>] 0) vsource type=sine freq=3M ampl=2.0
    v4 ([#bus<3>] [#/gnd!]) vsource type=sine freq=4M ampl=2.5

    Note that there is a bug in IC61X (CCR 752498) where this doesn't work in some cases. You need to use 

    envSetVal("asimenv" "mappingMode" 'string "oss")

    Before starting ADE. And you may need to do a Simulation->Netlist->Recreate to force it to renetlist after making the change. This changes the netlist mapping back to the IC5141 method (see http://support.cadence.com/wps/mypoc/cos?uri=deeplinkmin:ViewSolution;solutionNumber=11334086 )

    Note that the instance names are presumably not that critical, so you can call them whatever you want (they don't need to map to a bus name)

    Regards,

    Andrew.

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • Thodoros
    Thodoros over 14 years ago

     Andrew,

    Thanks for the responce on the specific issue which was quite helpful.

    I was worried some time now if we could use a bus rage (i.e. [#bus<0:15>]) in a stimulus file, or if there is a way of doing so. I understand that it is difficult for the analog to perform so, but if the bus is set to bit function could we use the range?

     

    Thanks in advance,

    Thodoros

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • Andrew Beckett
    Andrew Beckett over 14 years ago

    Hi Thodoros,

    Since the spectre language doesn't support buses (all the nets you see in the netlist are scalar) it doesn't really make sense to provide a whole bus (or even a multi-bit slice of a bus) such as [#bus<0:15>]. If you want to drive a vector, you should use the vector or vcd support in spectre which allows digital stimulus to be given. This is in the Setup->Simulation Files (VCD File, EVCD File, Vector File) in ADE.

    Regards,

    Andrew.

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • smthiid
    smthiid over 14 years ago

    Hello Andrew,

    I googled a lot to solve my question here http://www.cadence.com/Community/forums/p/18309/1260848.aspx#1260848, and found your post.  I think it may be helpful to use a vector file to generate the control signals for my 924 bits, but I don't know how.  I actually only need to set them to be either 0's or 1's, and I think if I can name them as [#bus<1:924>] and set a vector file it should work.  Could you please give me some guidelines?  Which manual should I refer to?

    Thanks,

    Tao

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
  • Andrew Beckett
    Andrew Beckett over 14 years ago

    Frank has given you the answer in your original question thread. Also, the format of the vector files is covered in the documentation (and "spectre -h vector" gives some good pointers).

    Regards,

    Andrew.

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information